Try saving a copy of the 'SRD_RELAY' from the 'Other Libs' to your **My Parts** folder. (**Open for Edit** then **Save**).

Not managing this - I've found the part (More Libraries .. search .. select .. Edit) but if I then save it asks me to create a new project and the part gets saved as a project not into My Parts. I tried it with the schematic part and the PCB Footprint part, I get the same result, a new project. Also which of the two components am I trying to put into My Parts, the Schematic Part or the PCB Footprint? What I'm trying to do is tell EasyEDA that when I create a board, this relay on the schematic (which I have managed to place) should be represented by a certain PCB Footprint part. Until I can make that connection, the board creation fails as the relay is shown as 'Error', I assume because it doesn't know what PCB Footprint part to use for it. I've been stuck on this simple task for a while, I'm clearly missing a basic concept.

seem to have started to figure this out - I managed to save the PCB Footprint as a My Part and then by naming the schematic part the same as the PCB part it was able to find it. Seems I did, even though the part was in a searchable library, have to add my own copy of the PCB Footprint to My Parts before this would work. I suspect I'm still getting something wrong here as the save prompted me to search for the part first in the same library which makes it seem like it should be able to find it. Sure there will be more as I learn this quite excellent tool. My first PCB is probably still a ways away at this rate.

Hi rols, Thanks for your like EasyEDA. Why you need to save it to your own? You need to confirm this package, and change, Maybe the PCB Footprints are created by others and not verified. EasyEDA footprints are in two types, 1. system, verify. 2 users contriubed, not veriyed. If you have time you can check http://easyeda.com/Doc/Tutorial/ out, there are lots of information that you can get.

Hi example - I'd rather not save the component to my own, I'd prefer to use them directly. In this case, yes, the components are User Contributed and not system. There's actually two, one schematic and one PCB Footprint. They are both user contributed. I can place the schematic one on my schematic, I can manually place the PCB Footprint one on a PCB, however I can't make the board generator generate a board from the schematic without first copying the PCB Footprint to My Parts. Is there a way I can 'confirm' or 'verify' the one in the library so I can use it without saving it to my own, or if it's a User Contributed one I need to save it to My Parts first? I've done most of the tutorial, it gives lots of information, but nothing about user contributed parts and how to use them. Also, the tutorial says that the 'Additional Libraries' section should have a Table of Contents on the left, but mine doesn't, it just has the search box. I wonder if the tutorial is for a slightly different version.

@rols, The safest way to build a PCB from a schematic is to save a copy of all the schematic symbols and PCB footprints that you are using in your design into **My Parts**. The footprints do not have to have the same name as the symbol but the name of your chosen footprint (package) must be associated with the schematic symbol in the schematic so that when you pass the schematic to PCB layout, the symbol in the schematic "tells" the PCB which footprint to pull out of My Parts. The schematic symbol does not have to have the same name as the PCB footprint because many different devices may have the same PCB footprint. However, when you choose a PCB footprint, you **must** check it *very* carefully against the manufacturers datasheet to ensure that the pinout of the footprint matches your chosen device. For instance the pinout of the 2N5457 and the, now obsolete, MPF102 jfet is the same but the pinout of the BF244 jfet is different even though they may be in the same TO-92 package. Most bipolar transistors are the same pin orientation in a SOT-23 package but some are not. The collector, base and emitter pin ordering of a bipolar transistor in a TO-92 package may be different from the Drain, Gate, Source pin ordering of a jfet or a MOSFET. Another example is that the PCB footprint for the TL084 opamp in a DIP 14 package is dimensionally the same as for the TL074 or the LM324 and has the same pinout but even though the PCB footprint for the LM3900 quad Norton amplifier or the LM339 quad comparator in a DIP 14 package is dimensionally the same as for the TL074, the pinouts are different. You can edit the pin ordering of a schematic symbol in the schematic by using the `I` Hotkey: >https://easyeda.com/Doc/Tutorial/introduction.htm#Hotkeys or: >**Super menu > Miscellaneous > Edit Symbol...** >https://easyeda.com/Doc/Tutorial/schematic.htm#PinmapModifysymbolinformation or select the part and then click the **Edit Symbol...** button in the right hand properties panel. ![Editing pin ordering using Edit Symbol...][1] When you first add a new part to the schematic, by using the `Add a parameter` button in the right hand properties panel, you can also add extra part attribute fields such as a brief `Description`, a `Supplier` and a `Supplier order code` and by ticking the `In BOM` box: ![Making added attributes show in the Bill of Materials][2] ![Adding attributes to help in BoM generation][3] those fields will then be added to the Bill of Materials when doing: > **Super Menu > Miscellaneous > BOM Report > BOM for Document...** These edits do not alter the library part but if you copy an edited part in the schematic to add more instances as required, then those edits will be copied too. (Oops! due to a missing feature in EasyEDA, whilst you can add extra parameters when you create a new part and save it to **My Parts**, these extra fields will not, at present (150806) actually appear in the BOM because there is no `In BOM` tick box!) Although it may be more time consuming to start with, you can make your life much simpler (and, because all the parts you create will appear in the publically searchable library, that of anyone who then searches for parts using the Search box and the Shift+F search) by creating symbols and footprints specifically for each part you use and giving the symbol and the footprint exactly the same name. You do not have to create a symbol or footprint from scratch: you can copy (clone) them from the library and just edit the names and pin ordering to suit your parts. * When you create parts, it is good practice to add sufficient information in the searchable part **Description** to allow users to see exactly what the symbol and footprint are for. ![Adding a searchable part Description that will appear in the Library][4] Note that this description information is separate from any Description field you may choose to add to the symbol that will apear in the schematic and BOM as described above. For example if you search for: >BC547 and then look under >**User Component** you'll find a BC547 symbol: https://easyeda.com/example/component/BC547-KTpHBTb5n and a BC547 footprint: >https://easyeda.com/example/component/BC547-FjdvNHmEy each of which is documented with a link to a device datasheet. Better still, if you search for: >BC547 TO-92 then, because Search also looks in the description text, almost the exact part will be found. For information on how to associate symbols and footprints please see the EasyEDA Tutorial: >https://easyeda.com/Doc/Tutorial/schematic.htm#ComponentAttributes For more information on pin ordering: >https://easyeda.com/Doc/Tutorial/prefix.htm#Schematicsymbols:prefixesandpinnumbers :) [1]: /editor/20150807/55c489f300bb4.png [2]: /editor/20150807/55c48469a27d7.png [3]: /editor/20150807/55c47e9c0471c.png [4]: /editor/20150807/55c48593bc9e9.png

Thank you for such a comprehensive answer, that must have taken forever. I definitely get the whole 'check the footprint' thing and have been doing so, the rest of the links will take me a while to read through but I'll do them all. At the end of this I shall have a PCB.

This is what we like! :)